Tran Thai Duong

These following notes and ideas are my personal experiments, may be wrong or not comfortable to you. So, just consider them references and feel free to discus.

1. Introduction

When working with ANSYS Classic, I prefer generate geometry models directly in ANSYS environment. Most of mechanical and civil models can be created using top-down or bottom-up style. Depend on the physic characters of real model; you must first decide which element type to use (beam, shell, solid …), then create corresponding FE model (lines, areas-surfaces, volumes). Good decisions will help reducing your time.

However, when you don’t want to use the ANSYS modeling or creating geometry models is not your part, it’s time for IGESs! IGES is the neutral format between CAD software and FEA programs. The most common situation is: one model but different purposes! Keep in mind that the IGESs you receive is not created for FE calculation.

So, after importing IGESs to ANSYS, there are many things to do before you can perform an FE analysis.

2. Some common problems when importing IGESs

–          The different tolerance between CAD software and ANSYS: This may cause undesired coincident keypoints, tiny lines, difficulties or fails when process Boolean Operations, …

–          Tiny, degeneracy entities (for example, a scratch left after Extrude cut): If you don’t check this carefully, your meshing may fail or you will get a extreme large number of nodes and elements, your results go wrong with stress concentration.

–          Separations of lines, areas and volumes: You may get a perfect mesh, but rigid body movement makes your solution fail. Even if you are lucky to have enough constrains, your simulations do not reflect true behaviors of you real structures.

3. Strategies to work with imported IGESs

3.1. Check your model carefully:

–          Before importing IGESs, you can set the tolerance:

Fig. 1: Set tolerance

–          Check for tiny, degeneracy entities: By using ‘Check Geom’, you can see if there was any.

Fig. 2: Check geometries

Determine your smallest dimension, then using ‘Sel Small Lines’, enter that value in SIZE field, check for region(s) that you doubt unwanted small features exist.

Fig. 3: Sel Small Lines

–          Check for Separations of lines, areas and volumes:

Plot line and exam the model, pan, zoom and rotate it! Here is an example for line model:

Fig. 4: Line model

In Fig. 4, you can notice 3 regions:

+) Region 1 and 2: Unwanted extra and shorten length. This is because of the tolerance or careless when drawing in CAD.

+) Region 3: lines are separated, the same color lines run across others. If lines are connected, you will see they are braked at joint keypoint and change their color.

Another example for solid model: You should set the ‘Numbering Control’ like Fig. 5.

Fig. 5: Numbering Controls

In Fig. 6, you can recognize that the volume (same color) run through others!

Fig. 6: Solid model

Now, plot line and notice how lines area arranged:

Fig. 7: Line mode

The lines are definitely not connected, so the areas and volumes at that position may be separated. Let’s try to delete that volume (delete volumes and bellow), you will see no trace of deleted volume on the left one!

Fig. 8: Delete volume.

3.2. Heal your model

After check for errors carefully, you can process fix what’s wrong. Use commands in Boolean Operations to divide, extend lines; glue areas, volumes; add some ones together if needed.

Sometime you must delete some entities then re-create them, remember this order: KP< LINE< AREA < VOLUME.

This step may cost a lot of time and experiments, so, be patient!

3.3. Mesh your model

You may generate a free mesh and let ANSYS do what it wants!

If you want a better mesh, here are some suggestions:

+) Consider the symmetric of your geometry, ex, if you want to mesh a solid circle, divide it into four, mesh one and take the SYMS twice.

+) If it is suitable for sweeping, just mesh the target area and sweep it.

+) Set suitable size (lesize, esize, …) for small angle, narrow corners, small entities.

+) Dive your model into simple parts that suitable for mapped mesh or sweeping (using WP, for example); mapped mesh or sweep first and free mesh for left parts, sometime you need to reverse this produce.

You can use this code to select volumes that can be mapped mesh:

NUMCMP,VOLU
alls
*get,vnum,volu,,count
*dim,vst,array,vnum
vs=0
*do,i,1,vnum
vs=VLNEXT(vs)
vsel,s,,,vs
aslv,s
*get,anum,area,,count
*if,anum,gt,6,then
vst(i)=vs
*endif
alls
*enddo

4. Conclusions

Importing and meshing an IGES is not a simple work if you want to get a good FE model. As you know, the quality of the mesh plays an important role in FE analysis, so the more careful you are the better results you get.

In recent revisions, AW has capacity to work well with IGESs and many other formats of CAD, it’s very fast and easy to import a geometry model created elsewhere and mesh it! But that’s another story!